Actions
Forum Thread Details
  • Replies 6 replies
  • Subscribers 176 subscribers
  • Views 862 views
  • Users 0 members are here
Related

Restring setting overrides pad size in library

autodeskguest

Hi all,

 

As far as I understand, the resulting restring size on the PCB will be the

largest of what's specified in the design rules and what's specified in the

library.

 

I use 35 % restring setting in my design rules. I have always done that, it

works fine and I would like to continue doing that. Now I'm faced with a

component that has two pins so close together that the pads will overlap

with a 35 % restring.

 

I have seen other PCB designs using this component. They have used elongated

pads with considerably smaller restring (in the narrower direction) to

prevent the pads from overlapping while still providing enough solder. When

I try changing the pad size in the library from auto to the necessary size

it is overridden by the 35 % setting in design rules.

 

Is there a way around this? Or is my only option to change the design rules

to, say, 15 % restring and then go into every single one of the other

through-hole mounted components I use in the library and set their pad sizes

to whatever they would have been with the 35 % setting? In that case, ouch.

 

//Christian

 

 

 

  •  

    Is there a way around this? Or is my only option to change the design rules

    to, say, 15 % restring and then go into every single one of the other

    through-hole mounted components I use in the library and set their pad sizes

    to whatever they would have been with the 35 % setting? In that case, ouch.

     

    //Christian

     

    Hi Christian,

     

    The goal in your situation is to modify the restring only as much as

    necessary to get the offending part to work. Usually, the effect on the

    rest of the components is acceptable. It's not often that a user has to

    go and change all of their other through hole components.

     

    In the current implementation of EAGLE restring is always in play, so

    things like this happen when you need really thin pads.

     

    hth,

    Jorge Garcia

     

     

  • in reply to autodeskguest

    In the current implementation of EAGLE restring is always in play, so

    things like this happen when you need really thin pads.

     

    hth,

    Jorge Garcia

     

    I was afraid of that. Unfortunately the component I want to use (a GbE PoE

    magjack) has the power output pins so close (1.48 mm pitch, 0.89 mm drill)

    that I would need to set the restring just below 25 %. That makes the other

    pads look really small, I'm afraid it will be a problem at least for hand

    soldering.

     

    I can't understand why the makers of those magjacks (Bel Fuse et al) have

    chosen to put those pins so close together, it's almost as if they intended

    them to be tied together. Not impossible, since only two of the four pairs

    in the Ethernet cable are supposed to be powered, but if they intended that

    then why would they provide four pins at all when two would have been

    sufficient. This perplexes me.

     

    Anyway, I guess there's nothing to do about this. I'll have to decide if I

    want to go with smaller pads across the board or if I want to go modify all

    the components in my library. Thanks anyway for the help.

     

    //Christian

     

     

     

  • You might be able to just make the pads in the library for that one part very small. When you insert it on the board the pads will be smaller than you want but will give you the electrical connection point. Then just connect with a wide wire or overlay the pads with polygons of copper, then place a circle (or whatever) in the soldermask layer to expose that part of the copper you want to be solderable. You might have to do the same in the solderpaste layer if you are going to make a stencil for soldering.

  • in reply to DonQ

    You might be able to just make the pads in the library for that one part

    very small. When you insert it on the board the pads will be smaller

    than you want but will give you the electrical connection point.

     

    No, that won't work. These are through-hole pads. I have to specify the

    correct drill diameter, otherwise I will have to manually edit the drill

    files after generating them. And with a given drill diameter, specifying a

    small pad size in the library doesn't help, since it will be overridden by

    the design rules' restring setting if that results in a larger pad.

     

    //Christian

     

     

     

  • in reply to autodeskguest

    Same answer, but instead of using thru holes in the library, use an SMD pad. In the layout, connect with a wire to the SMD connection point, then also insert a via at the connection point using the drill size you want. Then the via can have a restring diameter something different than AUTO, so make it what you want. If you then also need a long pad, or something different, you can either enter it as polygons in the library or directly on the board with polygons or wire segments.

     

    You may get DRC errors at this point, but it will be few enough that you can manually approve them.

  • in reply to DonQ

    Thanks, I can see that your suggestion would work, and that it would

    probably be better than the solution I arrived at.

     

    What I did was to make the drill size in the library smaller than it should

    be, so that the pad size came to be the one I wanted, and then I made sure

    that drill diameter was not included in the drill rack and increased the

    tolerance upwards so that the CAM processor had to chose the larger drill

    that I wanted.

     

    Of course this will only work as long as there are no other holes on the

    board that should be made with the smaller drill.